Calculation of hybrid joints used in modern aerospace structures
|
|
- Lynn Phelps
- 6 years ago
- Views:
Transcription
1 Calculation of hybrid joints used in modern aerospace structures Marcel STERE*,1, Daniela BARAN 2 *Corresponding author *,1 Aerospace Consulting, B-dul Iuliu Maniu 220, Bucharest , Romania sterem@incas.ro 2 INCAS - National Institute for Aerospace Research Elie Carafoli B-dul Iuliu Maniu 220, Bucharest , Romania dbaran@incas.ro DOI: / Abstract: The state of - the art of aeronautical structures show that parts are manufactured and subsequently assembled with the use of fasteners and/ or bonding. Adhesive bonding is a key technology to low weight, high fatigue resistance, robustness and an attractive design for cost structures. The paper results resolve significant problems for two groups of end-users: 1) for the aerospace design office: a robust procedure for the design of the hybrid joint structural components; 2) for the aeronautical repair centres: a useful procedure for structural design and analysis with significant cost savings. Key words: aircraft, hybrid joint, adhesive bonding, strap joint (single and double), FEA, ANSYS 1. INTRODUCTION Although they seem, at first sight very simple components, riveted joints actually have a great importance both in terms of flight safety and economic point of view. As for a modern transport aircraft, millions of rivets are utilized, they should receive a special attention with a view to their share in the total cost and, especially, in flight safety. Aloha flight is already a classic case which, because of the fatigue fracture of large areas of the fuselage (see Figure 1) has created a particularly situation with respect to the flight safety [7]. Figure 1 Fatigue Fracture of Boeing Fuselage Riveted Joints (combined with the effect of corrosion)., pp ISSN
2 Marcel STERE, Daniela BARAN 162 On April 28, 1988 a Boeing , flying the Hilo-Honolulu route (at an altitude of 7279 m) was severely damaged by fatigue fracture of a large section of the front fuselage. The plane was 19 years of service during which a multi-site damage occurred. The case represents a spectacular example of degradation by corrosion resulting in damage by fatigue during normal operation of the aircraft. An explosive decompression occurred and a piece of about 5.5 m of the cabin wall and structure behind the access door and above the passengers room separated from the aircraft. There were 89 passengers on board and 6 crew members. Seven passengers were seriously injured and a crew member was aspirated from on board. Then, there was an emergency landing on the island of Maui. A solution with visible effects on fatigue resistance and improvement of joining technology is the use of hybrid joints (bonding + riveting). The hybrid joint combines two methods, bonding and riveting, in order to provide more convenient properties than those obtained if each applies separately. Usually, after bonding and hardening of the adhesive, the bonded parts are drilled, after which the rivets are mounted. Compared to simple bonding, the hybrid assembling is more resistant to skinning (peeling), to static loading and impact stress, being also safer in operation and more resistant to variable stress. In relation to the simple riveting, the hybrid assembly offers the advantage of greater rigidity due to the continuity of the joint. 2. ISSUE STATEMENT Hybrid assembly (Figure 2) combines two methods, bonding and riveting, in order to provide more convenient properties than those obtained if each applies separately. A simple technology includes: surface preparation, application of the adhesive, metal plates drilling, installing of rivets (after the adhesive hardening). An important disadvantage is that fitting the rivets can dangerously damage the hardened adhesive. More secure is fitting the rivets immediately after applying the adhesive (still unhardened). Thus, hardening will occur with the parts assembled, maintained by the rivets in the correct relative position. That technique is easy to apply because there are adhesives with a sufficiently long (from 1:00 to 12:00). "Open time" (The time from applying the adhesive to the initial substrate to when it hardens effectively). For example, for epoxy adhesives, after fitting the rivets, curing may accelerate under the effect of temperature (by putting the assembled parts in the oven) [1]. Compared to simple bonding, the hybrid assembling is more resistant to skinning (peeling), to static loading and impact stress, being also safer in operation and more resistant to variable stress. In relation to the simple riveting, the hybrid assembly offers the advantage of greater rigidity due to the continuity of the joint. It is required to calculate the static behavior of a hybrid joint having junction plates either on one side or both sides (as in Figure 2).
3 163 Calculation of hybrid joints used in modern aerospace structures Figure 2 Hybrid assembly with junction plates on both sides Using a 2-D parametric model it is possible to achieve a sensitivity study [1] in order to highlight the influence of the following parameters on the stresses values of the adhesive layer: a) thickness of the adhesive, b) overlap length c) rigidity of the adhesive d) thickness of the adherents. 3. INPUT DATA In the study were considered: - Two types of adhesive: 1. Mono-component epoxy adhesive, AV 119 (ARALDITE 2007), with the tensile strength u = 70 MPa and the shear strength u = 47 MPa; 2. Two -component epoxy adhesive, Bison-metal, with the tensile strength u = 17 MPa and the shear strength u = 12 MPa; - Adhesives from aluminum alloy with the longitudinal elasticity modulus E Al = MPa and the Poisson constant Al = 0.33; - Rivets from aluminum alloy with the longitudinal elasticity modulus E nit = MPa, transverse contraction coefficient nit = 0.30, MPa, the shear strength u 125 MPa and the shear yield strength 0. 2 = 60 MPa. - Figures 3 and 4 show the characteristic curves for the aluminum alloy 2024-T3 and for the Bison - metal adhesive [1]. Figure 3 The characteristic curve for the aluminum alloy for the adhesive Bison-metal
4 Marcel STERE, Daniela BARAN 164 Figure 4 The tensile characteristic curve 2024-T3 Figure 2 shows the geometry of a join with junction plates on both sides, having the following dimensions: L mm, b=25 mm, t1 t2 t 1.6 mm, length of adhesive layer l a 2c mm and thickness 0.25 mm. The elastic parameters of the adhesive are: t a E 1250 MPa, a a 4. STATIC CALCULATION The static calculation can be done either using traditional engineering methods [2], [8], [9], [10] or using the finite element technology [ANSYS [3]) which offers wider and more precise ways to study this type of structure. The computing program utilized was ANSYS which has a rich library of finite elements that can model all types of joints that can be encountered in practice. First, a 2D calculation was performed to calculate the joint with adhesives. PLANE 82 element was used to model solid structures (PLANE 82 is best than PLANE 42 which also can be used). For the calculation of riveted joints as well as of the hybrid joints a 3D analysis will be performed and SOLID 92, TARGE170 and CONTA174 elements will be used. The element is defined by eight nodes having two degrees of freedom at each node: translations in nodal x and y directions (the element has the same capabilities as PLANE 42). For the 3D analysis SOLID 45 can be also used. SOLID 45 is defined by eight nodes (see Figure 6) having each three degrees of freedom at each node: translations in nodal directions: x, y and z. Figure 5 PLANE 82 Element
5 165 Calculation of hybrid joints used in modern aerospace structures Figure 6 Solid 45 Element SOLID 92 has a quadratic behavior and is very suitable for irregular networks.it also can tolerate irregular shapes without much loss of accuracy. The element is defined by 10 nodes (see Figure 7) each with three degrees of freedom per node: translations in nodal directions x, y and z. The element has many capabilities such as plasticity, creep, swelling, stress stiffening, large displacements and large deformations. Also, the element is able to include orthotropic material characteristics. Figure 7 SOLID 92 Element The unilateral junction plate model - figure 8 with PLANE 82 has 32,475 nodes and 10,616 elements while the bilateral junction plate model has 57,572 nodes and 18,915 elements. Due to its symmetry only half of the structure will be considered for the joint with a unilateral junction plate.
6 Marcel STERE, Daniela BARAN 166 Due to the symmetry against both axes of coordinates only a quarter of the structure can be used for the bilateral junction plate model.. Figure 8 2D Modelling with PLANE 82 For the bonded joints (without rivet) a 2-D model was issued with a finer mesh of the adhesive layer, adhesive-adherent interfaces and areas of stress concentration. Upper strip was guided horizontally (along the x axis) and subjected to force F b t, which induces a tensile stress o 10 MPa. TARGE170 element (Figure 9) is used to represent various 3D "target" surfaces for the associated contact elements (CONTA174). Target surface is discretized by a set of target segments (see Figure 9) are paired with associated contact surface via real constants set. Any translational or rotational displacement on the target segment element can be imposed. Forces and moments on target elements can also be imposed. For rigid target surface, these elements can be easily modeled in complex target forms (e.g. rivets). 1 o Figure 9 TARGE 170 Element
7 167 Calculation of hybrid joints used in modern aerospace structures CONTA 174 (Figure 10) is used to represent the contact and sliding between 3D target surfaces and a deformable surface of this element. The contact elements overlap the solid elements describing the boundary of the deformable body and are potentially in contact with the target surface (target) defined by TARGE170. The element is applicable to 3D structures and contact analysis at coupled fields. The element can be positioned on 3D solid surfaces or coated-type surfaces with knots in the middle of the sides (e.g. SOLID 92). The element has the same geometric features as the solid element to which it is connected. Figure 10 CONTA 174 Element The geometry and element nodes locations are shown in Figure 10. The element is defined by eight nodes (the solid over which it is placed has nodes in the middle of the sides). The order of nodes is consistent with solid nodes over which it is placed. 3D surface contact elements are associated with 3D target elements via the real constant set. The finite element model is designed so that it leads to a better approximation of the distribution of stresses in joint elements. In areas with high stress gradient (the extremity of the overlap section) the finite element mesh is refined. In the middle area of the joint (i.e. over 70% of the section overlapping the plate sheet-junction- plate) the stress distribution is approximately uniform. Thus the critical joint regions are those at the ends of the adherentadhesive interface. In addition, the adhesive thickness (where possible) is divided by a mesh of some elements in order to get the tensions variation on the adhesive thickness. Figure 11 The 3 D model of junction
8 Marcel STERE, Daniela BARAN 168 Figure 12 shows the plane model of a bonded joint, with a single junction plate (due to the symmetry only half of the structure has been modeled) and Figure 13 gives the spatial model of the hybrid junction plate joint (by bonding + riveting). Figure 12 Plane model for a bonded joint with a single junction plate Figure 13 Spatial model of a hybrid joint with junction plate The finite elements mesh was refined in areas with high stress gradient (ends of the overlap area). Figure 14 presents the variation of stresses in the median plane of the adhesive. One can find that joint critical areas are the extremities of the adhesive junction plate interface, an area where cracking will start, if the load reaches the limit value. The situation can be improved by using a junction -plate of variable thickness. Figure 14 Stresses distribution in the median plane of the adhesive 5. CONCLUSIONS Hybrid joints obtained by bonding and riveting, correctly made, have superior performance to those bonded. If bonding is performed first and rivets are mounted after the adhesive hardening, less resistant assemblies are obtained if compared with the case of rivets fixed before curing when more resistant junctions can be obtained.
9 169 Calculation of hybrid joints used in modern aerospace structures In this case the adhesive penetrates into the space between the rivet body and plate sheets and it hardens while the assembled parts are maintained by the rivets in the correct relative position [1]. The experimental result given in paper [1] on hybrid joints is very interesting. Figure 15 shows firstly the response of the joint when the rivet and adhesive are operating; then, when the adhesive broke, a sudden force decrease can be observed (supported only by rivets). Figure 15 Behavior of a hybrid joint In the design of the bonded and hybrid joints the main role is played by: - the material and thickness of adherents; - the thickness of the adhesive layer; - the adhesive flexibility. In case of joins with single or double junction plates, the best solution for reducing the stress peak at the ends of the overlap area is the use of junction- plates of a variable thickness. Also, the excess of the adhesive expelled under adherents can be modeled before hardening as a filler junction. REFERENCES [1] M. Sandu et al. Asamblari hibride cu adezivi si nituri la structuri din materiale compozite si aliaje de aluminiu (Proiectul ADENIT ). [2] L. Dorn, TALAT Lecture 4703 Adhesive Joints-Design and calculation, [3] ***, ANSYS 5.0 User s Guide,1992. [4] W. R. Broughton, G. Hinopoulos, Report No.15, Evaluation of the Single-Lap Joint Using Finite Element Analysis, Dec [5] S. Gomez et al., A simple mechanical model of a structural hybrid adhesive/riveted single lap joint, Int. J. of Adhesion &Adhesives, vol 27, pg , [6] ***, MIL-HDBK-5H Metallic Materials and Elements for Aerospace Vehicle Structures, 1 December [7] ***, Aloha Airlines, Official Accident Report Index Page, 04/28/88. [8] F. E. Bruhn, Analysis and Design of flight vehicle structures, Jacobs Publishers, N.,Suite 220, IN 46290, [9] M. R. Rivello, Theory and Analysis of Flight Structures, McGraww Hill Book, N.Y, [10] C. Y. Niu, Airframe Stress Analysis and Sizing, Conmilit Press Ltd., Wanchei Post Office, Hong Kong,1997.
Stress analysis of toroidal shell
Stress analysis of toroidal shell Cristian PURDEL*, Marcel STERE** *Corresponding author Department of Aerospace Structures INCAS - National Institute for Aerospace Research Elie Carafoli Bdul Iuliu Maniu
More informationCHAPTER 4. Numerical Models. descriptions of the boundary conditions, element types, validation, and the force
CHAPTER 4 Numerical Models This chapter presents the development of numerical models for sandwich beams/plates subjected to four-point bending and the hydromat test system. Detailed descriptions of the
More informationExample 24 Spring-back
Example 24 Spring-back Summary The spring-back simulation of sheet metal bent into a hat-shape is studied. The problem is one of the famous tests from the Numisheet 93. As spring-back is generally a quasi-static
More informationCOMPUTER AIDED ENGINEERING. Part-1
COMPUTER AIDED ENGINEERING Course no. 7962 Finite Element Modelling and Simulation Finite Element Modelling and Simulation Part-1 Modeling & Simulation System A system exists and operates in time and space.
More informationPrint Depth Prediction in Hot Forming Process with a Reconfigurable Die
Print Depth Prediction in Hot Forming Process with a Reconfigurable Die Jonathan Boisvert* Thibaut Bellizzi* Henri Champliaud Patrice Seers École de Technologie supérieure, Montréal, Québec *Master students,
More informationComputer Life (CPL) ISSN: Finite Element Analysis of Bearing Box on SolidWorks
Computer Life (CPL) ISSN: 1819-4818 Delivering Quality Science to the World Finite Element Analysis of Bearing Box on SolidWorks Chenling Zheng 1, a, Hang Li 1, b and Jianyong Li 1, c 1 Shandong University
More informationFINITE ELEMENT ANALYSIS OF A COMPOSITE CATAMARAN
NAFEMS WORLD CONGRESS 2013, SALZBURG, AUSTRIA FINITE ELEMENT ANALYSIS OF A COMPOSITE CATAMARAN Dr. C. Lequesne, Dr. M. Bruyneel (LMS Samtech, Belgium); Ir. R. Van Vlodorp (Aerofleet, Belgium). Dr. C. Lequesne,
More informationModeling and Simulation for Aircraft Structural Repair Using Modern FEA Tools
Modeling and Simulation for Aircraft Structural Repair Using Modern FEA Tools December 19-22, 2011 and January 9-12, 2012 Kuang-Hua Chang, Ph.D. Williams Presidential Professor School of Aerospace and
More informationRevised Sheet Metal Simulation, J.E. Akin, Rice University
Revised Sheet Metal Simulation, J.E. Akin, Rice University A SolidWorks simulation tutorial is just intended to illustrate where to find various icons that you would need in a real engineering analysis.
More informationCHAPTER 4 INCREASING SPUR GEAR TOOTH STRENGTH BY PROFILE MODIFICATION
68 CHAPTER 4 INCREASING SPUR GEAR TOOTH STRENGTH BY PROFILE MODIFICATION 4.1 INTRODUCTION There is a demand for the gears with higher load carrying capacity and increased fatigue life. Researchers in the
More information2: Static analysis of a plate
2: Static analysis of a plate Topics covered Project description Using SolidWorks Simulation interface Linear static analysis with solid elements Finding reaction forces Controlling discretization errors
More informationThrough Process Modelling of Self-Piercing Riveting
8 th International LS-DYNA User Conference Metal Forming (2) Through Process Modelling of Self-Piercing Riveting Porcaro, R. 1, Hanssen, A.G. 1,2, Langseth, M. 1, Aalberg, A. 1 1 Structural Impact Laboratory
More informationDesign and Analysis of Control Bay Used in Guided Missile
Design and Analysis of Control Bay Used in Guided Missile Ragam Prashanth 1, D.Muppala 2, Nirmith Mishra 3 1PG Student, Department of Aerospace, MLR Inst of Tech and Management, Hyderabad, Telangana, India
More informationSDC. Engineering Analysis with COSMOSWorks. Paul M. Kurowski Ph.D., P.Eng. SolidWorks 2003 / COSMOSWorks 2003
Engineering Analysis with COSMOSWorks SolidWorks 2003 / COSMOSWorks 2003 Paul M. Kurowski Ph.D., P.Eng. SDC PUBLICATIONS Design Generator, Inc. Schroff Development Corporation www.schroff.com www.schroff-europe.com
More informationReinforced concrete beam under static load: simulation of an experimental test
Reinforced concrete beam under static load: simulation of an experimental test analys: nonlin physic. constr: suppor. elemen: bar cl12i cl3cm compos cq16m interf pstres reinfo struct. load: deform weight.
More informationModelling Flat Spring Performance Using FEA
Modelling Flat Spring Performance Using FEA Blessing O Fatola, Patrick Keogh and Ben Hicks Department of Mechanical Engineering, University of Corresponding author bf223@bath.ac.uk Abstract. This paper
More informationANSYS Workbench Guide
ANSYS Workbench Guide Introduction This document serves as a step-by-step guide for conducting a Finite Element Analysis (FEA) using ANSYS Workbench. It will cover the use of the simulation package through
More informationChapter 3 Analysis of Original Steel Post
Chapter 3. Analysis of original steel post 35 Chapter 3 Analysis of Original Steel Post This type of post is a real functioning structure. It is in service throughout the rail network of Spain as part
More informationTechnical Report Example (1) Chartered (CEng) Membership
Technical Report Example (1) Chartered (CEng) Membership A TECHNICAL REPORT IN SUPPORT OF APPLICATION FOR CHARTERED MEMBERSHIP OF IGEM DESIGN OF 600 (103 BAR) 820MM SELF SEALING REPAIR CLAMP AND VERIFICATION
More informationFAILURE ANALYSIS AND OPTIMIZATION OF UNIVERSAL JOINT YOKE SUBJECTED BY TORSION AND SHEAR
FAILURE ANALYSIS AND OPTIMIZATION OF UNIVERSAL JOINT YOKE SUBJECTED BY TORSION AND SHEAR Avinash C Vasekar, Ranjitsinha R. Gidde, 1Research scholar, Department of Mechanical Engineering, SVERI s College
More informationComparison between Experimental and Simulation Results of Bending Extruded Aluminum Profile
ISSN 2409-9392,,, 2017,. 30 621.981.02 Naser M. Elkhmri, Budar Mohamed R.F. College of Engineering Technology Janzour, Tripoli, Libya Hamza Abobakr O. Technical College of Civil Aviation & Meteorology,
More informationX-FEM based modelling of complex mixed mode fatigue crack propagation
X-FEM based modelling of complex mixed mode fatigue crack propagation Hans Minnebo 1, Simon André 2, Marc Duflot 1, Thomas Pardoen 2, Eric Wyart 1 1 Cenaero, Rue des Frères Wright 29, 6041 Gosselies, Belgium
More informationATENA Program Documentation Part 4-2. Tutorial for Program ATENA 3D. Written by: Jan Červenka, Zdenka Procházková, Tereza Sajdlová
Červenka Consulting s.ro. Na Hrebenkach 55 150 00 Prague Czech Republic Phone: +420 220 610 018 E-mail: cervenka@cervenka.cz Web: http://www.cervenka.cz ATENA Program Documentation Part 4-2 Tutorial for
More informationModelling of an Improvement Device for a Tension Test Machine in Crippling Tests
Modelling of an Improvement Device for a Tension Test Machine in Crippling Tests Iván Lafuente *, José L. Alcaraz **, and Iñigo Ortiz de Zárate * * Dpto. de Cálculo. Aernnova Engineering Solutions. 01510
More informationCE Advanced Structural Analysis. Lab 4 SAP2000 Plane Elasticity
Department of Civil & Geological Engineering COLLEGE OF ENGINEERING CE 463.3 Advanced Structural Analysis Lab 4 SAP2000 Plane Elasticity February 27 th, 2013 T.A: Ouafi Saha Professor: M. Boulfiza 1. Rectangular
More informationISSN: ISO 9001:2008 Certified International Journal of Engineering and Innovative Technology (IJEIT) Volume 2, Issue 3, September 2012
Mitigation Curves for Determination of Relief Holes to Mitigate Concentration Factor in Thin Plates Loaded Axially for Different Discontinuities Shubhrata Nagpal, S.Sanyal, Nitin Jain Abstract In many
More informationGlobal to Local Model Interface for Deepwater Top Tension Risers
Global to Local Model Interface for Deepwater Top Tension Risers Mateusz Podskarbi Karan Kakar 2H Offshore Inc, Houston, TX Abstract The water depths from which oil and gas are being produced are reaching
More informationThe Role of Finite Element Analysis in Light Aircraft Design and Certification
The Role of Finite Element Analysis in Light Aircraft Design and Certification Nigel Bamber Wey Valley Aeronautics Ltd www.weyvalleyaero.co.uk Engineering Consultancy Civil and Military Aerospace and Motorsport
More informationTOPOLOGY OPTIMIZATION OF WING RIBS IN CESSNA CITATION
TOPOLOGY OPTIMIZATION OF WING RIBS IN CESSNA CITATION [1],Sathiyavani S [2], Arun K K [3] 1,2 student, 3 Assistant professor Kumaraguru College of technology, Coimbatore Abstract Structural design optimization
More informationFE ANALYSES OF STABILITY OF SINGLE AND DOUBLE CORRUGATED BOARDS
Proceedings of ICAD26 FE ANALYSES OF STABILITY OF SINGLE AND DOUBLE CORRUGATED BOARDS ICAD-26-43 Enrico Armentani enrico.armentani@unina.it University of Naples P.le V. Tecchio, 8 8125 Naples Italy Francesco
More informationANALYSIS AND OPTIMIZATION OF FLYWHEEL
Int. J. Mech. Eng. & Rob. Res. 2012 Sushama G Bawane et al., 2012 Research Paper ISSN 2278 0149 www.ijmerr.com Vol. 1, No. 2, July 2012 2012 IJMERR. All Rights Reserved ANALYSIS AND OPTIMIZATION OF FLYWHEEL
More informationUsing three-dimensional CURVIC contact models to predict stress concentration effects in an axisymmetric model
Boundary Elements XXVII 245 Using three-dimensional CURVIC contact models to predict stress concentration effects in an axisymmetric model J. J. Rencis & S. R. Pisani Department of Mechanical Engineering,
More informationPARAMETRIC STUDIES ON THE EFFECT OF FOUR TYPES OF FASTENER MODELING IN CHANNEL TYPE TENSION FITTING
PARAMETRIC STUDIES ON THE EFFECT OF FOUR TYPES OF FASTENER MODELING IN CHANNEL TYPE TENSION FITTING Venkata Geetha Urimila Siddabathuni 1, Srikanth Mekam 2, S S Subramanya Sastry 3 ABSTRACT 1 Team Leader,
More informationGENERALIZED MODELLING OF THE STABILIZER LINK AND STATIC SIMULATION USING FEM
ACTA UIVERSITATIS CIBINIENSIS TECHNICAL SERIES Vol. LXVIII 2016 DOI: 10.1515/aucts-2016-0004 GENERALIZED MODELLING OF THE STABILIZER LINK AND STATIC SIMULATION USING FEM COFARU Nicolae Florin professor
More information3D Finite Element Software for Cracks. Version 3.2. Benchmarks and Validation
3D Finite Element Software for Cracks Version 3.2 Benchmarks and Validation October 217 1965 57 th Court North, Suite 1 Boulder, CO 831 Main: (33) 415-1475 www.questintegrity.com http://www.questintegrity.com/software-products/feacrack
More informationEngineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering
Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Here SolidWorks stress simulation tutorials will be re-visited to show how they
More informationNumerical Validation of a Finite Element
Numerical Validation of a Finite Element GABRIEL JIGA, ANTON HADĂR, ŞTEFAN PASTRAMĂ, IOAN N. CONSTANTINESCU Department of Strength of Materials University POLITEHNICA of Bucharest Splaiul Independenţei,
More informationNUMERICAL DESIGN OPTIMISATION OF A COMPOSITE REACTION LINK
THE 19 TH INTERNATIONAL CONFERENCE ON COMPOSITE MATERIALS NUMERICAL DESIGN OPTIMISATION OF A COMPOSITE REACTION LINK Y. Yang*, C. Schuhler, T. London, C. Worrall TWI Ltd, Granta Park, Cambridge CB21 6AL
More informationRELIABILITY OF THE FEM CALCULATIONS OF THE FRACTURE MECHANICS PARAMETERS
International Conference on Economic Engineering and Manufacturing Systems Braşov, 26 27 November 2009 RELIABILITY OF THE FEM CALCULATIONS OF THE FRACTURE MECHANICS PARAMETERS Galina TODOROVA, Valentin
More informationA Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections
A Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections Dawit Hailu +, Adil Zekaria ++, Samuel Kinde +++ ABSTRACT After the 1994 Northridge earthquake
More informationFinite Element Buckling Analysis Of Stiffened Plates
International Journal of Engineering Research and Development e-issn: 2278-067X, p-issn: 2278-800X, www.ijerd.com Volume 10, Issue 2 (February 2014), PP.79-83 Finite Element Buckling Analysis Of Stiffened
More informationRevision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction
Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering Introduction A SolidWorks simulation tutorial is just intended to illustrate where to
More informationII. FINITE ELEMENT MODEL OF CYLINDRICAL ROLLER BEARING
RESEARCH INVENTY: International Journal of Engineering and Science ISSN: 2278-4721, Vol. 1, Issue 1 (Aug 2012), PP 8-13 www.researchinventy.com Study of Interval of Arc Modification Length of Cylindrical
More informationENGINEERING TRIPOS PART IIA FINITE ELEMENT METHOD
ENGINEERING TRIPOS PART IIA LOCATION: DPO EXPERIMENT 3D7 FINITE ELEMENT METHOD Those who have performed the 3C7 experiment should bring the write-up along to this laboratory Objectives Show that the accuracy
More informationCHAPTER-10 DYNAMIC SIMULATION USING LS-DYNA
DYNAMIC SIMULATION USING LS-DYNA CHAPTER-10 10.1 Introduction In the past few decades, the Finite Element Method (FEM) has been developed into a key indispensable technology in the modeling and simulation
More informationFinite Element Modeling and Failure Analysis of Roll Bending. Forming of GLARE Laminates
Finite Element Modeling and Failure Analysis of Roll Bending Forming of GLARE Laminates Jingming Tian, Gang Tao, Cheng Liu, Huaguan Li, Xian Zhang, Jie Tao* College of Materials Science and Technology,
More informationMSC/PATRAN LAMINATE MODELER COURSE PAT 325 Workbook
MSC/PATRAN LAMINATE MODELER COURSE PAT 325 Workbook P3*V8.0*Z*Z*Z*SM-PAT325-WBK - 1 - - 2 - Table of Contents Page 1 Composite Model of Loaded Flat Plate 2 Failure Criteria for Flat Plate 3 Making Plies
More informationANSYS Element. elearning. Peter Barrett October CAE Associates Inc. and ANSYS Inc. All rights reserved.
ANSYS Element Selection elearning Peter Barrett October 2012 2012 CAE Associates Inc. and ANSYS Inc. All rights reserved. ANSYS Element Selection What is the best element type(s) for my analysis? Best
More informationIntegrated FEM-based. package for Fatigue and Damage Tolerance - SAFE
Integrated FEM-based package for Fatigue and Damage Tolerance - SAFE Emmanuelle ALIOS Jean-Pascal KLEINERMANN 1 Content Introduction Airbus France tool : SAFE General overview Assessment of initiation
More informationStructural Analysis of an Aluminum Spiral Staircase. EMCH 407 Final Project Presented by: Marcos Lopez and Dillan Nguyen
Structural Analysis of an Aluminum Spiral Staircase EMCH 407 Final Project Presented by: Marcos Lopez and Dillan Nguyen Abstract An old aluminum spiral staircase at Marcos home has been feeling really
More informationES 128: Computer Assignment #4. Due in class on Monday, 12 April 2010
ES 128: Computer Assignment #4 Due in class on Monday, 12 April 2010 Task 1. Study an elastic-plastic indentation problem. This problem combines plasticity with contact mechanics and has many rich aspects.
More informationSolid and shell elements
Solid and shell elements Theodore Sussman, Ph.D. ADINA R&D, Inc, 2016 1 Overview 2D and 3D solid elements Types of elements Effects of element distortions Incompatible modes elements u/p elements for incompressible
More informationA MODELING METHOD OF CURING DEFORMATION FOR CFRP COMPOSITE STIFFENED PANEL WANG Yang 1, GAO Jubin 1 BO Ma 1 LIU Chuanjun 1
21 st International Conference on Composite Materials Xi an, 20-25 th August 2017 A MODELING METHOD OF CURING DEFORMATION FOR CFRP COMPOSITE STIFFENED PANEL WANG Yang 1, GAO Jubin 1 BO Ma 1 LIU Chuanjun
More informationSuper Elastic Alloy Eyeglass Frame Design Using the ANSYS Workbench Environment
Super Elastic Alloy Eyeglass Frame Design Using the ANSYS Workbench Environment Peter R. Barrett, P.E. Computer Aided Engineering Associates Inc. Patrick Cunningham Computer Aided Engineering Associates
More informationLOCAL STRESS ANALYSIS OF STIFFENED SHELLS USING MSC/NASTRAN S SHELL AND BEAM p-elements
LOCAL STRESS ANALYSIS OF STIFFENED SHELLS USING MSC/NASTRAN S SHELL AND BEAM p-elements Sanjay Patel, Claus Hoff, Mark Gwillim The MacNeal-Schwendler Corporation Abstract In large finite element models
More informationCHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING
113 CHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING 6.1 INTRODUCTION Superplastic properties are exhibited only under a narrow range of strain rates. Hence, it
More informationLearning Module 8 Shape Optimization
Learning Module 8 Shape Optimization What is a Learning Module? Title Page Guide A Learning Module (LM) is a structured, concise, and self-sufficient learning resource. An LM provides the learner with
More informationStress Analysis of Wing-Fuselage Lug Attachment Bracket of a Transport Aircraft
International Conference on Challenges and Opportunities in Mechanical Engineering, Industrial Engineering and Management Studies 162 Stress Analysis of Wing-Fuselage Lug Attachment Bracket of a Transport
More informationSTRENGTH ANALYSIS OF PIN CONNECTIONS USING COMPUTER AIDED SYSTEMS
STRENGTH ANALYSIS OF PIN CONNECTIONS USING COMPUTER AIDED SYSTEMS PETR BERNARDIN, VACLAVA LASOVA, FRANTISEK SEDLACEK University of West Bohemia in Pilsen RTI Regional Technological Institute Pilsen, Czech
More informationTHE COMPUTATIONAL MODEL INFLUENCE ON THE NUMERICAL SIMULATION ACCURACY FOR FORMING ALLOY EN AW 5754
THE COMPUTATIONAL MODEL INFLUENCE ON THE NUMERICAL SIMULATION ACCURACY FOR FORMING ALLOY EN AW 5754 Pavel SOLFRONK a, Jiří SOBOTKA a, Pavel DOUBEK a, Lukáš ZUZÁNEK a a TECHNICAL UNIVERSITY OF LIBEREC,
More informationMathematical simulation of riveting process
Mathematical simulation of riveting process Author: Margarita Kovtun E-mail: margarita_kovtun@inbox.ru Introduction he theme of this report arose in the context of the project which results from the cooperation
More informationA sizing method for cylindrical grid-stiffened structures in composite material
A sizing method for cylindrical grid-stiffened structures in composite material G. Gatta & F. Romano Structural Design & Aeroelasticity Laboratory CIRA - Italian Aerospace Research Center, Italy Abstract
More informationShell-to-Solid Element Connector(RSSCON)
WORKSHOP 11 Shell-to-Solid Element Connector(RSSCON) Solid Shell MSC.Nastran 105 Exercise Workbook 11-1 11-2 MSC.Nastran 105 Exercise Workbook WORKSHOP 11 Shell-to-Solid Element Connector The introduction
More informationStatic and dynamic simulations for automotive interiors components using ABAQUS
Static and dynamic simulations for automotive interiors components using ABAQUS Mauro Olivero, Vincenzo Puleo, Massimo Barbi, Fabrizio Urbinati, Benedetta Peyron Fiat Research Centre Giancarlo Luciani,
More informationEmbedded Reinforcements
Embedded Reinforcements Gerd-Jan Schreppers, January 2015 Abstract: This paper explains the concept and application of embedded reinforcements in DIANA. Basic assumptions and definitions, the pre-processing
More informationAufgabe 1: Dreipunktbiegung mit ANSYS Workbench
Aufgabe 1: Dreipunktbiegung mit ANSYS Workbench Contents Beam under 3-Pt Bending [Balken unter 3-Pkt-Biegung]... 2 Taking advantage of symmetries... 3 Starting and Configuring ANSYS Workbench... 4 A. Pre-Processing:
More informationANSYS AIM Tutorial Structural Analysis of a Plate with Hole
ANSYS AIM Tutorial Structural Analysis of a Plate with Hole Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Analytical vs. Numerical Approaches
More informationModule 1: Introduction to Finite Element Analysis. Lecture 4: Steps in Finite Element Analysis
25 Module 1: Introduction to Finite Element Analysis Lecture 4: Steps in Finite Element Analysis 1.4.1 Loading Conditions There are multiple loading conditions which may be applied to a system. The load
More informationTHREE DIMENSIONAL DYNAMIC STRESS ANALYSES FOR A GEAR TEETH USING FINITE ELEMENT METHOD
THREE DIMENSIONAL DYNAMIC STRESS ANALYSES FOR A GEAR TEETH USING FINITE ELEMENT METHOD Haval Kamal Asker Department of Mechanical Engineering, Faculty of Agriculture and Forestry, Duhok University, Duhok,
More informationSimilar Pulley Wheel Description J.E. Akin, Rice University
Similar Pulley Wheel Description J.E. Akin, Rice University The SolidWorks simulation tutorial on the analysis of an assembly suggested noting another type of boundary condition that is not illustrated
More informationStudy of Convergence of Results in Finite Element Analysis of a Plane Stress Bracket
RESEARCH ARTICLE OPEN ACCESS Study of Convergence of Results in Finite Element Analysis of a Plane Stress Bracket Gowtham K L*, Shivashankar R. Srivatsa** *(Department of Mechanical Engineering, B. M.
More informationmachine design, Vol.9(2017) No.1, ISSN pp
machine design, Vol.9(2017) No.1, ISSN 1821-1259 pp. 29-34 Research paper DYNAMIC ANALYSIS AND PARAMETRIC OPTIMISATION OF THE CONNECTING ROD USING AUTODESK INVENTOR Vasile George CIOATĂ 1, * - Imre KISS
More informationFinal project: Design problem
ME309 Homework #5 Final project: Design problem Select one of the analysis problems listed below to solve. Your solution, along with a description of your analysis process, should be handed in as a final
More informationSimulation of Discrete-source Damage Growth in Aircraft Structures: A 3D Finite Element Modeling Approach
Simulation of Discrete-source Damage Growth in Aircraft Structures: A 3D Finite Element Modeling Approach A.D. Spear 1, J.D. Hochhalter 1, A.R. Ingraffea 1, E.H. Glaessgen 2 1 Cornell Fracture Group, Cornell
More informationInfluence of geometric imperfections on tapered roller bearings life and performance
Influence of geometric imperfections on tapered roller bearings life and performance Rodríguez R a, Calvo S a, Nadal I b and Santo Domingo S c a Computational Simulation Centre, Instituto Tecnológico de
More informationStructural re-design of engine components
Structural re-design of engine components Product design cycle Design Development Testing Structural optimization Product knowledge Design freedom 2/18 Structural re-design of engine components Product
More informationA Computational Study of Local Stress Intensity Factor Solutions for Kinked Cracks Near Spot Welds in Lap- Shear Specimens
A Computational Study of Local Stress ntensity Factor Solutions for Kinked Cracks Near Spot Welds in Lap- Shear Specimens D.-A. Wang a and J. Pan b* a Mechanical & Automation Engineering, Da-Yeh University,
More informationNon-Linear Analysis of Base Plates in Automated Storage Systems
Non-Linear Analysis of Base Plates in Automated Storage Systems Ph.D. Juan José del Coz Díaz, Fco. Suarez Domínguez, Paulino J.Garcia Nieto University of Oviedo. Construction and Applied Mathematics Area.
More informationCHAPTER 5 FINITE ELEMENT METHOD
CHAPTER 5 FINITE ELEMENT METHOD 5.1 Introduction to Finite Element Method Finite element analysis is a computer based numerical method to deduce engineering structures strength and behaviour. Its use can
More informationDifficulties in FE-modelling of an I- beam subjected to torsion, shear and bending
DEGREE PROJECT, IN STEEL STRUCTURES, SECOND LEVEL STOCKHOLM, SWEDEN 2015 Difficulties in FE-modelling of an I- beam subjected to torsion, shear and bending MIRIAM ALEXANDROU KTH ROYAL INSTITUTE OF TECHNOLOGY
More informationThe part to be analyzed is the bracket from the tutorial of Chapter 3.
Introduction to Solid Modeling Using SolidWorks 2007 COSMOSWorks Tutorial Page 1 In this tutorial, we will use the COSMOSWorks finite element analysis (FEA) program to analyze the response of a component
More informationSimulation of Roller Hemming Process to Correlate the Design Parameters
Simulation of Roller Hemming Process to Correlate the Design Parameters Madhavi B. Raskar Student of Mechanical Engineering Department Sinhgad Academy of Engineering, Pune. Prof. S. C. Shilwant HOD of
More informationVehicle Load Area Division Wall Integrity during Frontal Crash
Vehicle Load Area Division Wall Integrity during Frontal Crash H. Türkmen TOFAS Türk Otomobil Fabrikasi A.S. Abstract : This study addresses design efforts of a vehicle load area division wall and the
More informationNEW WAVE OF CAD SYSTEMS AND ITS APPLICATION IN DESIGN
Vol 4 No 3 NEW WAVE OF CAD SYSTEMS AND ITS APPLICATION IN DESIGN Ass Lecturer Mahmoud A Hassan Al-Qadisiyah University College of Engineering hasaaneng@yahoocom ABSTRACT This paper provides some lighting
More informationExercise 1: 3-Pt Bending using ANSYS Workbench
Exercise 1: 3-Pt Bending using ANSYS Workbench Contents Starting and Configuring ANSYS Workbench... 2 1. Starting Windows on the MAC... 2 2. Login into Windows... 2 3. Start ANSYS Workbench... 2 4. Configuring
More informationCHAPTER 7 BEHAVIOUR OF THE COMBINED EFFECT OF ROOFING ELEMENTS
CHAPTER 7 BEHAVIOUR OF THE COMBINED EFFECT OF ROOFING ELEMENTS 7.1 GENERAL An analytical study on behaviour of combined effect of optimised channel sections using ANSYS was carried out and discussed in
More informationAUTOMATED METHODOLOGY FOR MODELING CRACK EXTENSION IN FINITE ELEMENT MODELS
AUTOMATED METHODOLOGY FOR MODELING CRACK THEME Structural Analysis - Durability, Fatigue & Fracture. James J. Kosloski Senior Engineering Manager - CAE Associates Dr. Michael Bak Senior Engineering Manager
More informationChapter 1 Introduction
Chapter 1 Introduction GTU Paper Analysis (New Syllabus) Sr. No. Questions 26/10/16 11/05/16 09/05/16 08/12/15 Theory 1. What is graphic standard? Explain different CAD standards. 2. Write Bresenham s
More informationFatigue design of welded bicycle frames using a multiaxial criterion
Available online at www.sciencedirect.com Procedia Engineering 34 (2012 ) 640 645 9 th Conference of the International Sports Engineering Association (ISEA) Fatigue design of welded bicycle frames using
More informationPerformance Evaluation of Finite Elements for Analysis of Advanced Hybrid Laminates
Performance Evaluation of Finite Elements for Analysis of Advanced Hybrid Laminates Hemanth R. H, Ruchin P, Gourav G, Venkatesha K. S and Ravi Kumar, G. V. V Infosys Technologies Limited, Electronic City,
More informationDetermination of the solicitation types responsible for the deformed. shape of an aircraft cockpit
Determination of the solicitation types responsible for the deformed shape of an aircraft cockpit Infante, V. 1*, Gomes, E. 1 and Branco, C.M. 1 1 Departamento de Engenharia Mecânica, Instituto Superior
More informationLesson 6: Assembly Structural Analysis
Lesson 6: Assembly Structural Analysis In this lesson you will learn different approaches to analyze the assembly using assembly analysis connection properties between assembly components. In addition
More informationIMPROVED SIF CALCULATION IN RIVETED PANEL TYPE STRUCTURES USING NUMERICAL SIMULATION
26 th ICAF Symposium Montréal, 1 3 June 2011 IMPROVED SIF CALCULATION IN RIVETED PANEL TYPE STRUCTURES USING NUMERICAL SIMULATION S.C. Mellings 1, J.M.W. Baynham 1 and T.J. Curtin 2 1 C.M.BEASY, Southampton,
More informationAnalysis of Detroit Seismic Joint System
Analysis of Detroit Seismic Joint System for EMSEAL Corporation Prepared by Haig Saadetian, P.Eng. Senior Consultant ROI Engineering Inc. 50 Ronson Drive, Suite 120 Toronto ON M9W 1B3 26-April-2009 1 Contents
More informationLinear Elastic Fracture Mechanics (LEFM) Analysis of Flaws within Residual Stress Fields
Linear Elastic Fracture Mechanics (LEFM) Analysis of Flaws within Residual Stress Fields David Woyak 1, Brian Baillargeon, Ramesh Marrey, and Randy Grishaber 2 1 Dassault Systemés SIMULIA Corporation &
More informationAnalysis of Composite Aerospace Structures Finite Elements Professor Kelly
Analysis of Composite Aerospace Structures Finite Elements Professor Kelly John Middendorf #3049731 Assignment #3 I hereby certify that this is my own and original work. Signed, John Middendorf Analysis
More informationWP1 NUMERICAL BENCHMARK INVESTIGATION
WP1 NUMERICAL BENCHMARK INVESTIGATION 1 Table of contents 1 Introduction... 3 2 1 st example: beam under pure bending... 3 2.1 Definition of load application and boundary conditions... 4 2.2 Definition
More informationFinite Element Method. Chapter 7. Practical considerations in FEM modeling
Finite Element Method Chapter 7 Practical considerations in FEM modeling Finite Element Modeling General Consideration The following are some of the difficult tasks (or decisions) that face the engineer
More informationAdvanced Finite Element Model for AE-MDB Side Impact Barrier
Advanced Finite Element Model for AE-MDB Side Impact Barrier Authors: M. Asadi 1, P. Tattersall 1, B. Walker 2, H. Shirvani 3 1. Cellbond Composites Ltd. 2. ARUP Campus (UK) 3. Anglia Ruskin University
More informationWORKSHOP 6.3 WELD FATIGUE USING NOMINAL STRESS METHOD. For ANSYS release 14
WORKSHOP 6.3 WELD FATIGUE USING NOMINAL STRESS METHOD For ANSYS release 14 Objective: In this workshop, a weld fatigue analysis on a VKR-beam with a plate on top using the nominal stress method is demonstrated.
More information